Macros and Renishaw Probe

Hola Folks,

I'm currently running some aluminum prototypes for a new medical customer, which could turn into a massive job (which is what they all say, I know...) I have one bore that is 2 inches deep that I needs to be 1.6000-1.6006 . That's plenty of room as far as I'm concerned, once I get the bugs worked out. However, just wondering if any programming gurus know if I could run the part, probe the bore, have the machine look at it's info on the size of the bore, and if the bore is undersized to have it run another skim pass, or to beep at me and call me a jerk if the bore is over sized. I'm not really looking for specifics, just "Sure, one can do that if one know's what one is doing..." or "No, The Haas software isn't up to that task."

That is it. Use T in the bore cycle to update the tool offset with the adjusted diameter. An incremental adjustment will be made to your "wear" offset, so if you have it run the tool over, it will compensate accordingly.

G65 P9814 D1.6003 H.0003 T8 This will measure your nominal size, H is tolerance, and T is tool that will be updated once measured.

If the bore is out of the tolerance specified, then the probe will automatically freeze there with an alarm. (generic probe stop with an out of tolerance alarm)

There is also simple code you can write to re-run the bore, or alarm at a different line of code but from your first question, I will keep it simple, as per your request.

Hey Matt, I could really use that manual, too. I have been trying to figure out how to customize some probe routines, and have been having a few issues...
My e-mail is ryehoon[at]gmail[dot]com. Thanks!

probe manual

Hi Matt. I was wondering if you could send me that manual too. I have recently had a Renishaw probe installed on my VF2ss, but I'm having some trouble getting started. email is sdcy99@ymail.com. If you can send it, I would really appreciate it. Thanks

I think if I was going to try to hold a bore within .0006 I would be using a boring head with G76 Cycle.
You could still probe the bore if you wanted too. If you have the newer Haas control you can change one of the parameters
so it actually reports the last measurement the probe made as one of the items on the screen.
You will probably use .0003 of your tolerance with out of roundness. Especially 2" Deep.
Nothing like a nice round bore

This has probably already crossed everyone's mind, but I would make sure that when the program is complete and the hole is sized that you don't allow the wear comp to stay the same.

If you are running in the afternoon and then shut it down until next morning, the growth in the machine will be different and could possibly scrap a part.

At the beginning of the program I would maybe include a macro variable to clear the wear offset as a safety precaution. Although I don't know if probing each part and re cutting will kill your production time.

Or if you run 24/7 the constant adjustments would make this a non issue unless there is a break in production for some hours.

HAAS parameters

Originally Posted by MachEng

I think if I was going to try to hold a bore within .0006 I would be using a boring head with G76 Cycle.
You could still probe the bore if you wanted too. If you have the newer Haas control you can change one of the parameters
so it actually reports the last measurement the probe made as one of the items on the screen.
You will probably use .0003 of your tolerance with out of roundness. Especially 2" Deep.
Nothing like a nice round bore

Can you remember parameter number? Is a 2011 controller consider as newer? Thanks